Endmills

Endmills are cutting tools designed so as to be able to cut in the X- and Y- axis when mounted in a spindle. Some are also able to cut when plunging along the Z-axis (Centercutting), while others cannot (Non-centercutting).

One consideration for endmills is the tolerance to which they are made and how the actual diameter relates to the nominal diameter. Arguably the best way to handle this is to cut a slot or a shape and measure the result, but one may wish to start by measuring the endmill itself (doing so in such a way as to avoid damaging the delicate cutting edges[1]), esp. if one is using a spindle w/ very low runout.

There is a direct correlation between price and quality and tool longevity. While one should not expect a cheap bit to perform well, one also should not spend excessively on high-end bits when first beginning, given the possibility of destroying the bit through accident or mis-use.

Collets and endmills must be kept clean, any foreign material will increase runout and may lead to breakage.[2]

Endmills should be installed as deeply as is needed in a spindle collet, (in accordance with the manufacturer guidelines so as to not cause "overcolleting") with this reduced so as to increase projection only so much as is needed to cut the deepest feature in a given job (and no less than the manufacturer's guidelines recommend). For light cuts, 3/8" should be considered the absolute minimum which is inserted.

Acronyms

Every specialty these days tends to develop its own special terminology and acronyms. Machining from which CNC derives is no different, but for the most part, endmill terminology is straight-forward, at least to folks accustomed to working in a shop. That said, there are some acronyms which may be confusing, these are noted (and explained) below.
c.f., the Glossary

LOC: Length of Cut so basically how much of the end mill has a cutting area on it

FL or FOL: Flute Length - Length of flutes or grooves.

OAL: Over all length or how long the bit is in total from one end to the other.

End Mill Selection Guidelines

All other things being equal:

Length

Shorter endmills are more rigid, less-expensive and may provide a better finish (as a corollary, one should expose only the length of endmill beyond the cutting edge which is absolutely necessary[4])

Longer endmills, while not as rigid, afford the ability to cut more deeply, are more expensive and may not provide as nice a finish and may increase runout (see above note)

Number of flutes

One, two or three flutes are esp. suited for slotting or heavy stock removal

Four or more flutes provide a nicer finish and greater tool rigidity

Diameter

Larger diameter tools are more rigid and will clear more material in a given pass

Smaller diameter tools will have a smaller radius at corners and allow one to remove less material when profiling or cutting out parts, resulting in less waste and fewer chips. This may have safety implications.[5]

The best starting point is the default 2-flute, square-ended, straight-cutting (able to center-cut) 1/8" high speed steel (or solid carbide) endmill w/ no coatings.[7] One should move away from that baseline as is dictated by the materials which you are cutting, and the fashion in which you wish to mount them in the work-area, and the quality of cut which you expect. Switching to a spiral up-cut endmill for better chip ejection is an obvious choice (to the detriment of cut quality and increased chipping at the top surface when cutting plywood).

Suggested starter set

Note that endmills are consumables, and one pretty much has to have at least 3 for any sort you're going to be relying on:

Forum Discussions

Shapeoko 3

If one is starting with just a 1/4" collet:

three 2-flute 1/4" straight endmills (such as the #201 endmills from Carbide 3D --- one will be included with the machine, a pack of two will fill one out with: 1 for initial experimentation/roughing, 1 for finishing passes, and 1 spare

two 2-flute 1/4" ball end endmills (such as the #202 endmills from Carbide 3D) --- if one wishes to do 3D modeling or cut parts which have rounded profiles along the bottom (often a good idea in woodworking for increased strength)

two 90 degree V-bits such as the #301 from Carbide 3D --- if one wishes to do V-carving or cut joints which use this angle

Add the 1/8" endmills from the above SO2 section if getting a 1/8" collet for detailed work.

Custom Endmills

Note that it is possible to have an endmill made to order if there are not any stock options which suit.

High Speed Steel (HSS)

High speed steel is commonly used when a special tool shape is needed, not usually used for high production processes, but since it will hold a sharper edge than carbide may be used for finishing passes for crisper edges and possibly more accurate dimensions. Inexpensive, at the cost of tool life, though resilient and often used for aluminum, but has a far narrower cutting speed range than carbide.[10]

Cobalt (M-42: 8% Cobalt)

An improvement over high speed steel. Reduced chipping under severe cutting conditions allowing the tool to run faster than HSS.

Powdered Metal (PM) Cobalt

Cost-effective alternative to solid carbide.

Solid Carbide

Able to run much faster than other materials, carbide is especially well-suited to use with rotary tools for general usage. Incredibly tough and long-lasting, it is brittle and subject to chipping, so should be handled with care. Carbide inserts are the most common because they are good for high production milling.

Carbide-Tipped

Usually used to make large-diameter tools.

Geometry

An End Mill cutter with two flutes

Depending on the material being milled, and what task should be performed, different tool types and geometry may be used. For instance, when milling a material such as aluminium, it may be advantageous to use a tool with very deep, polished flutes and a very sharp cutting edge. When machining a tough material such as stainless steel, however, shallow flutes and a squared-off cutting edge will optimize material removal and tool life.

Non-optimal geometry will create results similar to a dull bit, e.g., fuzzy cuts in softer species of wood. Making a final finishing pass may help (w/ a HSS bit if possible), another alternative is to spray a clear finish on the wood, allow it to dry and then re-run the finishing pass (the sprayed finish will soak into the wood and harden it).

End mills are described using a number of characteristics:

Shape

The most frequently used shapes are Square End (Flat) and Bell-End endmills.

Square

Square End (Flat)--- general purpose, will cut a slot with squared off bottom

Fishtail --- The tips of the cutting edge extend down past the center of the bit, making it especially suitable for punching through thin materials or cutting fine details[11]

Radiused

Radiused (Bull Nose[12])--- general purpose, has corners slightly radiused so as to not cut a perfectly square corner at the bottom of the cut (see below)

Ball-end

Ball-End --- general purpose, will cut a slot with a rounded bottom. The radius will result in a stronger part, and will allow for more control over the shape of a pocket, but will require a large step-over value to avoid a scalloped appearance.

Stepover

V-bits

V-cutting --- special purpose, used for engraving or chamfering, or cutting parts w/ angled sides. Identified by the angle of the V --- 90 degree bits can be used for mitering. Sharper angles will cut deeper for a given width of cut. Engraving bits with a single-flute (look like half cones) are able to cut more deeply w/ a single pass.[15] Most V-bits are unable to clear chips, so require slower speeds.[16] See also V-carving reference books.

# of Passes --- Size guidelines for adding a radius at the tip (may vary based on bit angle and material):

<10mm --- one pass

10--20mm --- ~0.5mm

20--35mm --- ~0.75mm

>35mm --- 1mm radius

The tradeoff is feature size vs. feature depth --- an acute angle allows one to cut a smaller, finer feature w/ more depth, while a more obtuse angle allows one to cut a larger area w/ a single pass and while having a single bottom, as opposed to a ragged set of scallops.

Recommended bit angle for a given text size:

<1" 45--60°

1--2" 60°

2--4" 60--90°

4--6" 90°

6--10" 90 to 120°

>10" 120° or greater

Material guidelines:

hardest timber available

use conservative plunge and feedrates even when doing more than one pass

avoid overlapping V-cuts --- tends to cause splintering at the top edge, leave a ~0.5--1mm gap at the top

use a cutter w/ centered/symmetrical geometry

Formula for calculating the effective diameter of a V-bit at a given depth in Excel this is:[17]

Note that the angle of a given endmill may vary slightly, esp. if it has been resharpened. One suggested technique is to prepare a series of files set to V-bits at different angles and cut them in a piece of scrap so as to determine which angle best suits a given endmill.[19] Images along with a link to a Vectric post: http://www.cncnutz.com/2017/06/test-your-v-bit-angle-episode-151.html

Also available are tapered endmills which shape the cutter into a triangular shape (usually between 0.5 and 15 degrees) so as to increase rigidity

End Cut Types

Centercutting --- one or more cutting edges at the tip to allow plunge, drill or ramp movement into a cut. Most flexible, best-suited for general-use.

Non-Centercutting --- only capable of side (radial) cut or contour cutting into an exterior surface. Special-purpose, only suited for applications where plunge cutting is not necessary.

Similarly, flute geometry is available in several different forms:

Straight --- general purpose cutting (wood or plastic[21]) --- will not cause as much chipping at the top as an up-cut spiral

Spiral

up-cutting --- pulls up on the work-piece, pulls the bit and the machine down into the cut --- affords the best possible chip ejection --- may cause chipping at the top surface on some materials[22]

down-cutting --- pushes the work-piece down, and won't lift up thin materials --- poor chip ejection may result in re-cutting of waste material, dulling the bit, cleaner top edges on shallow pockets[23]

combination --- (also known as Compression) bottom portion of the cutting area is up-cutting and the upper portion is down-cutting, resulting in a better edge finish in materials which chip easily such as plywood. Requires that one be able to make a cut in a single pass for best results. Similarly, the total cut depth must be deeper than the transition point.[24] See https://www.youtube.com/watch?v=E9MmOxVlNwM

Spiral cutting flutes may also vary in their geometry by the angle at which the helix works its way up the shaft of the tool (Variable Radius[25]). Shallower angles are used for roughing, while sharper ones are used for tooling intended to create a fine finish.

Endmills are also described by the shape of the flutes for some designs, e.g., O-flute.

Comparison to drills

Note that the cutting geometry for endmills is optimized for cutting horizontally, one guideline on this is that an endmill is 4x better at cutting along XY than a drill, while a drill is 4x better at plunge cutting vertically along -Z. Note that some CAM programs will build this consideration into their generation of paths, and so will require that holes be ~10% larger than the diameter of the endmill. This has implications for the surface, so will require a finishing pass.[26]

Number of Flutes

Single Flute

Largest possible flute space allowing for the greatest possible chip carrying capacity. Used for aluminum and plastics on commercial machines, is well-suited for plastics on less-rigid equipment.

Two Flute

Largest possible flute space in a symmetrical design. Used primarily in slotting and pocketing of non-ferrous materials where chip removal is a concern on commercial machines, is well-suited for general usage on less-rigid equipment.

Three Flute

Similar flute space to two flute designs, but having more material and greater rigidity.

Four/Multiple Flute

Used for peripheral and finish milling on commercial machines. The additional flutes allow faster feed rates, but chip removal may be problematic. Provides a much finer finish than tools with three or fewer flutes.

Flute shape

Various shapes and soakings afford differing capabilities, mostly related to chip clearing, but also to reduce chatter.[27] In general, deeper flutes afford better chip clearing (suited for wood and plastics), while shallower flutes make for a more rigid tool and are better for harder materials (metals).

Flute Length

The length of the flutes will determine how much of the endmill can be engaged in cutting. There is a trade-off between longer cutting length and rigidity of the endmill. Normal cutters will have a flute length of three times their diameter. Stub length endmills will have shorter cutting area while extra long cutters will have more.

Longer flutes also allow the machine to make deeper cuts without rubbing, and to take full depth finishing passes.

Note that it is important to not insert endmills so deeply in a collet that the cutting edges are in contact with the collet. Always follow the manufacturer guidelines for min. and max. depth of insertion.

Coatings

In the early 1990s, use of coatings to reduce wear and friction (among other things) became more common. Most of these coatings are referred to by their chemical composition, such as:

PCD veins. Though not a coating some endmills are manufactured with a 'vein' of polycrystaline diamond. The vein is formed in a high temperature-high pressure environment. The vein is formed in a blank and then the material is ground out along the vein to form the cutting edge. The tools can be very costly, however can last many times longer than other tooling.

Milling Formula

Revolutions per Minute (RPM): Number of revolutions the endmill makes in a minute

Inches per Minute (IPM): Number of inches the endmill passes through the workpiece in one minute

Chip Load: The amount that each flute cuts during a single revolution of an endmill

Surface Feet per Minute (SFM): This is the cutting speed of the endmill. It is
the number of feet per minute that a given point on the circumference of a cutter travels per minute

Mounting an endmill

Follow the spindle manufacturer's instructions. Some users of low-end rotary tools with problematic collets have reported success using a bit of plumber's Teflon thread tape or some other material.[33] It would be preferable to get a replacement collet (or tool).

Collet and Endmill Size

Note that collet and endmill shaft size must match (though ER and ER-style collets have a fairly broad clamping range). Consult your manual if you have any questions or concerns, and follow the router/spindle manufacturer's guidelines.

Total Indicated Runout Considerations

Another consideration is the interplay between bit diameter and the TIR (Total Indicated Runout) of a given spindle. If it is a significant portion of the end mill's diameter, the possibility of breakage increases significantly. Unfortunately, rotary tools often suffer from significant lack of concentricity in their bearings and other internals which often increases with wear/usage (see the Spindle Options page for further information and other options).

Maintenance and Usage

While one must view endmills as a consumable item, they are also a fine piece of tooling. It is possible to sharpen certain endmills (but the companies which do so have a rather large minimum quantity for doing so). Another possibility is the old shop tradition of using used tooling for rougher work, or materials which do not require the same sharpness, then switching to a newer, sharper tool for a finishing pass.[35]

Don't mix tools: e.g. a tool used for aluminum should not be used for wood - the aluminum residues blunt the cutting edges and increase friction.[36]

Recycling

High Speed Steel and Carbide are both welcome at recyclers and should be carefully recycled once one has a sufficient quantity of material to make a trip worthwhile.

Carbide Processing will pay for used carbide tooling in suitable quantities.

Specialty shapes

Note that for specialty bit shapes, one will need either a CAM tool which supports said shape (as of this writing, the only extant tool which does so is a commercial one for dovetail bits), or be willing to draw or hand-code suitable paths.

Ogee

Ogee bit --- 1mm depth passes and slow the speed way down around 300--400 mm/min[107]